Manufacturing

Weldment Design with Autodesk Inventor 6

1 Nov, 2002 By: Jeff Wymer


Inside the recently released Autodesk Inventor 6 is a weldment-design environment. It allows you to design the weldment assembly, as well as weld-bead specification, weld-edge preparation, and post-weld machining. You can use the drawing manager inside Inventor 6 to create drawings that document the entire weldment-manufacturing process, from component drawings to pre-weld drawing views and post-machining views. Special 2D symbols allow for both automatic and manual creation of standards-based welding drawings. This complete workflow of 3D design to 2D documentation ensures that all the design information captured in 3D transfers automatically to the 2D drawing.

Welding
To begin, we need to enter into the welding environment. This can be accomplished in two ways: by taking an existing Autodesk Inventor assembly and converting it into a weldment by using the "Applications" pull-down and selecting "Weldment" or by creating a new weld design by selecting the "Weldment" template.

When converting an existing Autodesk Inventor assembly, you will be prompted to enter the standard you want to use (ISO, ANSI, and so forth) and the weld-bead material. When starting a new weld assembly by using the weld template, you will not be prompted for these variables. By default, the standard will be the one chosen during installation. To set the default weld-bead material type, you can edit the weldment template file. Select Document Settings from the Tools pulldown, and select the Weld properties tab.

These two weldment variables may be changed at any time by simply choosing Document Settings to change the standard. To edit the weld-bead specification, simply right-click on the welds feature in the browser and choose properties.

On entering the weld environment, you will notice the panel bar has changed to the weldment-design icons and the assembly browser has updated to include new environments: Preparations, Welds, and Machining, as shown in Figure 1.

figure
Figure 1. The new weld design tool palette and feature browser allows for preparations, welds, and machining operations to be fully defined within the assembly file.

Within these environments are the operations or tasks you need to complete. For instance, by double-clicking on Preparations, you will be placed into the preparations environment. This will allow you to prep the parts before welding by adding chamfers, holes, cuts, and so on. All of the preparation features will be maintained and managed here. Any preparation added in the weldment environment lives in the assembly/weldment level; it doesn't exist at the part level. For example, if you add a chamfer or a cut to clean up raw stock before welding, it is documented within this weldment-assembly file and does not show up in the individual part file.

By double-clicking on the Welds, your environment will change to let you add welds to your assembly. Again, the browser and panel bar will update to this environment automatically. Inventor allows for two types of welds to be applied to the model: cosmetic and fillet weld. Cosmetic weld creates a weld feature that annotates edges in the weldment, but does not add weld-bead geometry. Fillet weld creates a fillet weld feature with 3D geometry that represents a physical weld bead.

When using the fillet-weld option, the 3D weld is illustrated with a texture map so non-designers can visually understand the 3D geometry, as shown in Figure 2. In order to see this, you will need to enable Show Reflections and Textures in your program options. By using the 3D fillet weld feature, you can perform interference checking between the weld beads and other parts. You will also be able to retrieve information such as volume and mass by calculating mass properties on the welds. This will allow for very accurate weld weights and center of gravity calculations of your welded assemblies. To access mass properties of the weld feature, simply highlight the "Welds" in the browser, right-click, and choose properties.

figure
Figure 2. Complex fillet welds can be applied to an assembly with weld symbology automatically created and displayed in 3D.

Cosmetic welds allow for all weld options, including fillet, seam, spot, flange, and so on. When using cosmetic, you won't see a visual weld feature--it will simply highlight the edge orange where the weld is placed. Cosmetic welds allow for faster performance on complex weld assemblies by not carrying the 3D-feature data.

Regardless of whether you choose the cosmetic or fillet-weld option, you will always have the 3D-weld annotation placed on the model. This allows for easier documentation during the weld-drawing process and eliminates costly errors during the documentation phase. And in the future, other applications0 could be enabled to see and use these 3D annotations. Programs such as Autodesk Streamline will currently let non-designers see weld annotation and make queries.

Machining
The Machining environment lets you add post-weld machining. The features created here are similar to preparations, where they only exist within this weldment assembly--not at the part file level. Valid machining features are Extrudes, Holes (including tapped holes), and Chamfers.

Inventor is intelligent enough to know that when you enter into preparations or machining, you are removing material not adding it. Therefore, it automatically doesn't allow you to select join or intersection. This alleviates any possible errors that may find their way to the shop floor.

figure Figure 3. When creating drawings of the weldment-assembly file, new options allow you to select which weld environment to document: Assembly, Preparations, Welds, or Machining.

Documenting
Inventor lets you document the entire weld process by easily extracting all information from the 3D-weld assembly. During the create drawing-view process, there is a new option in the dialog box that allows you to select what type of drawing view to create: assembly, preparations, welds, or machining, as shown in Figure 3. When creating drawing views, you can use the new Options tab in the dialog box. It defines the drawing view options during creation. There are several new display options as well, such as automatic centerlines, work planes, weld symbols, and weld annotation. By choosing weld annotation, Inventor will automatically illustrate all fillet welds as solids and caterpillars. When you choose the Weld Symbols option, Inventor will place the weld symbols on the drawing file automatically.

I would recommend creating a weldment drawing template to include multiple drawing-sheets so all the process welding sheets are created automatically. To do this, simply open the standard.idw file located in the templates sub-directory under install. Next, right-click in the browser background and select "New Sheet." I would now recommend creating the number of drawing sheets to follow your documentation process of weldments. Save this drawing file as weldment.idw in your template directory. Now, when you create a new file, you will see weldment.idw as a new template, and this will automatically include all the process sheets necessary to fully document your design.

Inventor 6 allows you to define and document your weld processes by using its new task-based weld environment. It lets you define preparations, welds, and machining operations contained within one assembly file. This information can then be documented in the drawing environment. This allows you to work in a natural workflow that is familiar to the actual weldment-manufacturing process.


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